Trying to drill some holes in A36 steel plate. using a Precision twist drill, 11mm looks to be a heavy web split point, M42. 1/4" plate through holes. It drilled one and broke on #2.
Per the ME consultant I was using 787 rpm and 6.38 IPM
I did two peices in 10 gauge steel with a 6mm drill and the drill went through but it did bow the plate.
I'm thinking I need to switch to standard point drills. Which means I need to go to equivilent decimal sizes. or should I drop the feed rate down?
What you've got isn't actually a drilling setup. It's a custom made, spring loaded drill breaking device. Works every time.
Here's what's happening. Your speed and feedrate are about right, and they work out to around .008" per rev, sorta. But the drill doesn't really cut .008 deep with each rev. What it does is cut maybe .004 or .006 per rev, at the same time it's causing the plate to bow by .002 or .004. This continues (often with chatter when the drill's just starting) until the plate has bowed as much as it can or will. That happens when the force required to bow it any more becomes equal to the force that the drill needs to feed and cut. From there on, until the point of the drill breaks out on the other side of the plate, things proceed as you might expect.
But when the point DOES break out, then the drill breaks off. As soon as the chisel point on the drill gets through the other side of the plate, the infeed force created by the drill drops by a LOT. Like 50% maybe. Which means the drill is suddenly NOT pushing hard enough to keep the plate bowed like it was when the point was still pushing like crazy.
So, the plate springs back, and unbows itself. And your chip load gets HUGE in a hurry. Instead of .008 per rev, you now get .008 PLUS the movement of the plate as it straightens itself out. That can be .020, or .030, or just about anything. And this is happening AFTER the point of the drill is through the hole, and when the drill is making contact with the plate only with its corners, and with the outermost parts of its cutting edges. When the feedrate goes crazy, the cutting edges bite, hard, and then the drill untwists itself and turns to junk.
Simple.
(The reason you got away with this kind of thing in the 10 gauge steel is that something that thin isn't strong enough to spring back like the 1/4" stuff. The force from the drill's cutting edges - even without the chisel point - was still more than the workpiece could match, so the grab-and-bite action didn't happen until the drill was almost completely through the hole. Then, the drill only had to grab and bite a little bit at its corners. Good drills will often survive that, but I'm told they don't enjoy it much.)
Here's how you fix things: First, support the plate you're drilling. Put something thick and rigid underneath it - really underneath ALL of it - and drill into a sacrificial sub-plate. That keeps the plate you're drilling from bowing away from the drill. Most of the time, that solves the problem. Also, you need to use a drill whose point is split right down to almost nothing. That minimizes the chiseling and pushing action, and lets the drill act like a cutting tool, rather than a bulldozer, everywhere except at the thiniest little bit of its center. The reduction in pushing force can be quite dramatic, and so can the reduction in the work wanting to bow and warp and do crazy little dances.
If I understood you correctly, you're now using some kind of split point, but are thinking about switching to a "standard" point, presumably with a wider chisel. That's exactly the wrong way to go, and it will make your problem worse.
In some cases, like when a drill is really sharp, a thin plate will actually lift TOWARD the drill as the point breaks through. The drill (once the point is no longer cutting) will work like an auger, and will pull on the plate, which will also cause a sudden increase in chip load just as the chisel point quits cutting. The solution for that is to clamp the plate well, as near as possible to the places where you're drilling. In extreme cases, a rigid sacrifical plate is even placed ON TOP of the workpiece, in addition to the one underneath; and the drill goes through three pieces of metal to make the desired hole in just one of them.
i UNDER STAND COMPLETELY WHAT YOU ARE SAYING, BUT, ALTHOUGH MY PEICE IS A36 PLATE STEEL IT IS ONLY CUT ,damn caps lock. 3.15" wide x a little over 5" long. sitting on parallels in my vise. can't flex that much in 3".
10 gauge plate was 3.35" wide.
I did finish with a standard drill. I got me some weird pointed drills that need tons of thrust to go in. I'll need to see if I can find a PTD company catalog around here and see if I can find these drills, maybe they are non-ferrous only?
.008" per revolution?? For a 1/4" drill? A bit steep, IMO. And 51.5 sfm seems a bit slow, but then I've never cut A36.=20
Couldn't find anything on A36 specifically, but Machinery's Handbook shows surface speeds for carbon steels to be anywhere between 15 to
130 sfm. So maybe you've got it right where it should be.
I'd back off on the feed. That's a rather small drill to be feeding that fast. Getting it down to .002 - .003" IPR (which would be 1.57" to 2.36" for you IPM guys), along with flood coolant, will certainly help with the breaking problem.
PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here.
All logos and trade names are the property of their respective owners.